Need Help!- Fadal won't Z home at program end

[rdoty]

My program goes to Z-home for tool changes without a problem but I can't get it to stop at Z-home at the end of the program. It always goes above by the amount of the fixture height which causes the machine to do an E-stop.

I've tried several program endings with no success.

Here's the last few lines of code:

N47 M5 M9
N48 G0 G90
N49 G53 Z0
N50 M6 T9
N51 G0 G90 X-.44 Y0 E3 S4000 M3
N52 H9 Z0.8 M8 P2000
N53 G1 Z0.3 F10.
N54 Z0.8
N55 X0.22 Y-0.381
N56 G1 Z0.3 F10.
N57 Z0.8
N58 X0.22 Y0.381
N59 G1 Z0.3 F10.
N60 M5 M9
N61 G0 G90
N62 G53 Z0
N63 M6 T10
N64 H10 Z0.8 M8
N65 G84 G99 R0+1. Z0.425 F200.2 Q0.03125 P50 X-0.44 Y0 E3
N66 X0.22 Y-0.381
N67 Y0.381
N68 M5 M9
N69 G80 Z5.0
N70 G0 X0 Y5.
N71 M30

I had the same problem with all tool changes before I inserted G0 G90 followed by G53 Z0 and then the head would go to Zhome, do the tool change and proceed.

When I ended the program with G0 G90 and G53 Z0 and M30 the head would go above Zhome and fault.

Then I read that the sub-routine needed to be canceled which should be G80 so I added G80 Z5.0 and the Y move and M30, which I think should stop the program and wait until I reload a part then load the first tool but it doesn't. I'm baffled because all the other tool changes followed by G0 G90/G53 Z0 go to Zhome. What am I missing?

[txcncman]

Soooo...why don't you end the program with:

G0 G91 G28 Z0
G0 G90 X0 Y5.
M30

I do not think Fadal will do G53. You can try E0 though.

[rdoty]

Thanks. That works.....sort of.

I'm beginning to think my machine is possessed.

That works except at the very end....the head retracts to Z home, the table moves to the front and then........the head drops down a little, taps one more hole in thin air, and retracts to 0.47 below Z home where it waits patiently for me to recycle, which happens normally.

If you have an answer (I'm even open to exorcism) that's great. As for me I'm off to make parts.

Thanks again for your help.

[txcncman]

What happened to the G80 Canned Cycle Cancel? Did you take it out?

G80 should come immediate when you want canned hole making cycles to end.

[angelw]

Originally Posted by rdoty Thanks. That works.....sort of. I'm beginning to think my machine is possessed. That works except at the very end....the head retracts to Z home, the table moves to the front and then........the head drops down a little, taps one more hole in thin air, and retracts to 0.47 below Z home where it waits patiently for me to recycle, which happens normally. If you have an answer (I'm even open to exorcism) that's great. As for me I'm off to make parts. Thanks again for your help.

The fact that the control executes another tap cycle, means that the Tap Canned Cycle (Fanuc parlance, Fadal call Canned Cycles Fixed Cycles) has not been canceled. Fadal Fixed Cycles are canceled with G80. After the last coordinate at which the Fixed Cycle is to execute has been programmed, program G80 as shown in the fix of your listed program example to cancel the Fixed Cycle.

N65 G84 G99 R0+1. Z0.425 F200.2 Q0.03125 P50 X-0.44 Y0 E3
N66 X0.22 Y-0.381
N67 Y0.381
N68 G80
N68 M5 M9

The P address may be used to increase or decrease the feed rate out of the hole in a Fixed Tapping Cycle. Use a positive P to increase and a negative P to decrease the feed rate out of the hole. The P address is specified in terms of percentage of the Feed In Rate. Accordingly, in your example P50 would be +50% of the In Feed Rate. Depending on the depth of the hole being tapped and the amount of extension available with the Tap Holder being used, this much increase of feed rate may give you grief.

Sorry txcncman, you Posted whilst I was typing my answer.

Regards,

Bill

[nash398]

would G30 Z0 work just befor the M30

[angelw]

Originally Posted by nash398 would G30 Z0 work just befor the M30

No G30 with the Fadal Control. G28 will work.

Regards,

Bill

[rdoty]

Sorry I didn't respond last week...

I did forget to put the G80 back in. Works wonders when you cancel the subroutine!
Also, angelw, you are correct that P50 might cause me grief. I think I originally wanted P5, not P50. Only broke one tap! Small tap (6-32) so it only went PINK!

I spent some time yesterday (Sunday) going over the program speeds and feeds and discovered that my seat-of-the-pants guestimates were off in the wrong direction. I need to slow down!